DriveWorksXpress in SolidWorks 2008 (Solid Thinking SolidWorks Tutorial)

30 Apr, 2008 By: Richard Doyle

This integrated tool enables you to create infinite variations of a model using rules-based projects that you set up one time and run over and over again.

Design automation has always been a hot topic, especially for companies that produce many variations of one product. Rules-based design automation has been around for a long time, but usually at a price — time and money. So SolidWorks has partnered with DriveWorks to provide DriveWorksXpress, a tool that is integrated with SolidWorks.

Using Rules-Based Automation
DriveWorksXpress helps automate your design processes. With DriveWorksXpress, you can create infinite variations of a model using rules-based projects that you set up one time and run over and over again. The simple examples below represent only a fraction of what you can do with DriveWorksXpress.

Getting Started with DriveWorksXpress
DriveWorksXpress is already integrated inside of SolidWorks, so you don't need to select it as an add-in. When working in a part or assembly, DriveWorksXpress is accessible on the Evaluate tab of the CommandManager.

The DriveWorksExpress icon.

Let's start with a simple assembly model consisting of a couple of flanges and a shaft and throw in some locating pins for good measure. The goal is to create separate models and drawings based on the size of the shaft. Using DriveWorksXpress, you'll set up a project that will allow you to create different variations of the assembly based on the shaft size. You'll also use the project to decide on the number of locating pins (one or three). Finally, you'll automatically create drawings for each new model.

Setting up a Project
The first step is to set up a project. Select the DriveWorksXpress icon from the CommandManager to start the DriveWorksXpress wizard. Select the Create/Change Database radio button and click Next. Enter a file name for the new database in the dialog box.

The DriveWorksXpress wizard.

Once the database is created, it's time to add the models. Click the Add Models radio button and then click Next. There are different options for adding models to the database. If the model is already open in SolidWorks, use the default Use Current Open Model radio button. Otherwise, you can Browse for a new model. Click Next.

The DriveWorksXpress dialog box shows the structure of the model in a tree format. Here you'll select the models to control. Since you're creating new models based on the size of the shaft, you'll also have to control parameters for the parts the shaft passes through. Select the shaft, collar, and rigidhub parts in the tree. Click Next.

Capturing parts.

The next step is to capture dimensions, features, properties, and drawings that will be used to create the new variations of the models. In this example, you need to change bore diameters to match the change to the shaft, a circular pattern feature to change the number of pins, and the existing drawings that will be the basis for the new drawings. Starting with the flange assembly selected, click the Drawing tab to browse for the drawing. In this example, you'll also create a new drawing for the collar. Repeat the steps to capture the existing drawing for the collar.

Next you'll capture the required dimensions and features. Click back to the Dimensions and Features tab, and select the shaft from the tree. The shaft part is displayed in the SolidWorks window. Click Add.

Capturing features and dimensions.

The DriveWorksXpress wizard disappears, and you are taken to the SolidWorks window, where the shaft part is displayed. The DriveWorksXpress property manager appears below the SolidWorks FeatureManager Design Tree.

The DriveWorksXpress Property Manager.

Here you'll capture the dimension for the diameter of the shaft. Double-click on the part to display the feature dimensions (or turn on the display of annotations in the FeatureManager Design Tree). Select the .500 diameter dimension, enter a DriveWorks name in the dialog box (here it's called ShaftDiameter), and click Apply. The dimension is captured and is listed under Dimensions in the Captured Information dialog box. You can repeat this step to capture as many parameters as needed. Click Finish to return to the DriveWorksXpress wizard. Repeat these steps to capture the bore diameter on the collar and rigidhub parts. Since the plan is to also drive the number of locating pins in the assembly, you will need to capture the hole feature and the derived pattern to drive the parameters. DriveWorksXpress recognizes these as features and adds them to the list.

At this point, you have enough information captured to start creating your variations. DriveWorksXpress can also capture customer properties that can be modified by using rules, but for the purposes of this article, let's skip that step. Click Next.

Creating Forms
The next step is to create a custom form to set up the requirements for new variations of the models. The first thing to do is to create a parameter that will drive new model names for each variation. Click Add and type in the name of the project (I used Project). Select Text Box as the type, and make sure the Required checkbox is checked. Next, add fields to allow input for other parameters. In this example, I'll allow shaft diameters of .25" to .50" in increments of .06". In the Name box, enter Shaft Diameter and select Spin Button from the pulldown menu. At the next dialog box, enter the minimum, maximum, and increment values in the appropriate fields.

Setting up a form.

The next requirement to set up is the number of pins in the collar part. For that, you'll control whether the circular pattern in the collar part and the derived pattern in the flange assembly are suppressed or unsuppressed (effectively controlling the number of pins). From the Form dialog box, click Add. In the name field, use NumberofPins, and set the Type to Drop Down. A new dialog box appears, allowing you to add a set of different selections — add 1 and 3. Click Next.

Setting up Rules
Now that you have the parameters, you need to set up rules to determine what happens when you changed them. The Rules Summary dialog box gives an indication regarding what is needed. If you're going to create new parts and drawings based on parameter changes, you'll need to create file names for them. Likewise, you need to tell DriveWorksXpress what to do with certain features and/or dimensions that are affected by parameter changes. Click Edit All Rules, and then click Next.

Rules Summary dialog box.

To set up a rule for the file names, double-click the top level model in the Rule Editor dialog box. A second dialog box opens and you can begin to add rules. For the file name rule, you'll capture input from the form you set up using the Project parameter. Select Input, then Project to add the file name rule. Repeat this step for all of the other models. When finished, click Next to return to the rules list.

The Rules Editor.

Move on now to the dimension rules. Since the shaft passes through the collar and rigidhub, you have to set up rules to control the diameters in each part. In this example, you'll assume that the diameter for the rigidhub is a slip fit, and the diameter for the collar is a press fit. Click Edit Dimension Rules, and then click Next.

Double-click on the shaft to display the Rules Editor dialog box. DriveWorksXpress uses logic to help produce the desired values. For the shaft part, use input from the forms to determine the value. Select Inputs, and then select ShaftDiameter (the parameter you added to the form). Click Next to return to the model list. Next you'll set up the rule for the different bore sizes you need. Double-click the collar part. From the Logic pull-down, select the = sign, then select ShaftDiameter from the Inputs pulldown. Finally, from the Math pulldown, select the – sign, and then add a value in the dialog box. The rule should look like the one below.

Adding dimension rules.

Dimension rule for collar bore.

Repeat this step for the rigidhub part, but instead of a value of -.0005, use a value of +.002 for the ShaftDiameter parameter.

The last rule to set up is the number of pins in the collar part. For this, once again use input from the form you created. Click Edit Feature Rules, and then click Next. Using the Logic pulldown, and the Numberofpins input, set up the rule (=IF( NUMBEROFPINS = 1 , "SUPPRESS" , "UNSUPPRESS"). Click Next. The rules summary should now show that all rules are defined. Click Next.

Running the Project
The final step is to complete the input form and run the project to create the new variations. Type in the name of the project (I used ONE-QUARTER-SHAFT), select the Shaft Diameter (0.2500), and the Number of Pins (1). Click Next.

Add the parameters.

Now comes the fun part, watching DriveWorksXpress work its magic. A dialog box appears that shows you everything that is happening behind the scenes. You can also watch as the new models and drawings are created. When DriveWorksXpress is finished, a dialog box displays with the results.

The DriveWorksXpress results.

New models and drawings were created to reflect the change in the shaft diameter, as well as bore diameters specified, and a new assembly model. New drawings were created to reflect the number of pins.

DriveWorksXpress is a great tool for design automation. You can create multiple variations of your design using an easy wizard interface. New part models, new drawings, and new assemblies are generated based on the rules and parameters you set up. Once a DriveWorksXpress database is set up, use it over and over again to drive new derivations of your designs.

For more information about DriveWorksXpress, including some terrific tutorials and videos of DriveWorksXpress in action, visit the DriveWorksXpress Web site.

About the Author: Richard Doyle

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